Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
Thanks for all the replies guys. I realise I was not very detailed in my post, preferring to pose the question in general terms. The actual circuit I have is as follows. 1 L298 H-bridge driving a stepper motor. The driver is controlled by an L297 stepper motor controller. This generates the phase sequence & PWM for the driver. The 'Ground' end of the H-bridge is connected to ground through a current sense resistor. The net connecting the H-bridge to the current sense resistor is the 3mm wide one. The motor current passes through this net and the sense resistor to ground, hence the need for a wide trace. The purpose for the sense resistor is to give current feedback to the PWM generator. Routing the wide traces back to the L297 for feedback is not really an option. The sense input on the generator is an opamp input. I don't know if it is bipolar or not. Given that only short distances (>6cm total for the line from sense resistor to the opamp input) are involved I can use a thinner trace (0.35mm). There is no separate ground sense line. This configuration has worked fine for me in the past. When I route a board I usually setup the width constraint for each net, autoroute the board and then manually cleanup. In this case the auto router will route the net using the 3mm thickness throughout. If the part of the net which did not have to be so wide could have its width defined seperatly, then the autorouter would route differently and probably better. The virtual short thing sounds interesting & I can see how it works. I'm less sure how the from-to width rule works never having used it. Thanks for all the feedback. Joe * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
At 11:10 PM 9/3/2003, Ian Wilson wrote: It is common to have four connections to a current sense resistor, two on each side. One on each side will be big and fat to carry the current, and the other with be a signal trace (carrying no current) that ensures the voltage drop across just the resistor is sensed - the voltage drop across power tracks, ground planes etc are ignored. They are ignored because they are irrelevant. This kind of arrangement is used with some kind of differential amplifier (or bridge, I suppose), so the current will be equal to the differential voltage divided by the sense resistance, quite accurately, it will be as accurate as the resistance. However, in some circuits it might be possible to ignore the ground leg drop. For example, the ground connection might be through a ground plane, and the sense amplifer circuitry is referenced to this same plane I'm not describing all the details and possibilities... (do I hear a sigh of relief? :-) The only tricky stuff with this is that it requires common-mode input ranges beyond, or at least close to, the supplies in many situations - but this is no longer rocket science. Normally the sense resistor, as I've seen it, is in the return, as in the matter at hand. So if, for example, we have high voltage to the load, we don't need to deal with high voltages in the current-measurement circuitry, we are only dealing with voltages close to ground, well within the instrumentation supply voltage. Of course, if the fabricator opens up that virtual short, we're likely to have a fairly spectacular error indication * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
At 10:43 PM 9/3/2003, JaMi Smith wrote: [in the original inquiry it was stated:] > >I need to have a current return line with 3mm thickness. "return" generally refers, in my experience, to the wiring which returns to ground or other more negative voltage. I'm sure someone can come up with a more precise definition. But it might be used, in this case, to refer to the return line coming from the load, not to ground, but to a sense resistor and from there to ground or common. The sense resistor is of a low value, and the voltage drop created by the current through it will be small compared to the voltages involved in driving the load. [...] > >This line connects to a current sense resistor. I need to take a line from > >this resistor to an amplifier input. The writer did not state which side of the resistor is connected to the amplifier input. The imprecision of the question has led to a bit of confusion in the answers, but it does not really affect the most important part of the answer, only the dicta. Since the writer only refers to one sense line, I'm assuming that the voltage drop in the current path from the resistor to ground may be neglected; otherwise one would need to use *two* sense lines and a differential amplifier, though it might also be possible to calibrate the circuit and get away with only a single sense line. In other words, the true sense resistor would be the assembled part plus the resistance of the remainder of the ground circuit. Quite clearly, however, the inquirer was concerned with a voltage sense line and its different width requirements from what is otherwise the same net, Iret. Perhaps the "amplifier" is located on the other side of the circuit board, or even on another circuit board. [I wrote:] > Presumably there will be negligible current in the sense line (the > "amplifier input line.") At least whatever measures that voltage should be > designed to minimize the current. So the line can be narrow, really it only > needs to be wide enough to be reliably fabricated. > I would disagree here, in that I believe that the trace should be large enough to not contribute any "losses" of its own by being so narrow that differences in manufacturing runs may produce traces which may have differences in their own resistivity, which will in fact affect the circuit. Mr. Smith must be having a bad day. (Or I've really lost it myself, certainly a possibility) The resistivity of this line in a current measurement application will have no effect on the voltage at the amplifier, since, in a properly designed circuit, there will be no current in the trace. If there is no current, there is no voltage drop. True, if the current is rapidly varying, resistance could create some problem, but it would be unlikely in a normal power application for this to be an issue. There needs to be a good direct path from the "load" side of the current sense resistor back to the input of the amplifier, and it needs to have no problems of its own such as losses or crosstalk from other circuits. Crosstalk might be an issue, I suppose, but, again, in power circuitry, it would be unusual for the problem to be such that a bit of capacitance at the amplifier input would not eliminate it. We might be talking DC, here. If crosstalk is an issue, I'd think the thickness of the trace might be irrelevant If we are talking RF, all bets are off. Assuming that "Iret" is in fact the "return net" from the "load", Yes, I'm sure that's what he meant. He's free to chime in with a correction, of course! and is a large trace connected to one end (the "load" end) of the current sense resistor, with the other end of the current sense resistor being connected to ground (the negative supply), Yes. It's a large trace for heat reasons, less likely losses might be an issue. But losses in the Iret trace will not affect the current measurement if the sensing point is right at the high end of the sense resistor. Drop in the ground end net *would* be an issue, though it might be possible to ignore it, as was implied by the question. I would say that there should be another trace going from the same "Iret" end of the current sense resistor to the amplifier input. "Another" trace? That's the trace he was asking about! Perhaps Mr. Smith intended to refer to a trace from the ground end (not the "Iret" end) of the sense resistor, which would then be used in a differential voltage measurement, i.e., a differential amplifier would be used. But this was not the question we were asked. However, the trace size and naming and DRC issues would be the same, only it would be with two traces instead of one. This trace is the "feedback" portion of the "Iret" trace, or what I would call the "feedback" trace, but there is absolutely no reason in the world that this trace should have a different "net" name, or have any "virtual short" involved with it. I must say that Mr. Smith has lost me here. "feedback"? F
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
- Original Message - From: "Ian Wilson" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Wednesday, September 03, 2003 8:10 PM Subject: Re: [PEDA] Joining 2 different nets keeping seperate identifiers? > On 12:43 PM 4/09/2003, JaMi Smith said: > >There are basically two different ways that a current sense resistor is > >normally used. The first is between a voltage source and a "load", and the > >second is between the "load" and ground. In both cases, the voltage drop is > >measured across the current sense resistor between the supply leg and the > >"load". > > > I think, Jami, that you are missing a critical aspect or it is getting > buried in too much verbage. Sorry if I have just missed it, I am afraid I > am doing you something of a disservice by not reading your post(s) in full. > You are right in that sometimes I can get too longwinded in trying to explain someting, and I really need to try and just keep it short and simple. > It is common to have four connections to a current sense resistor, two on > each side. One on each side will be big and fat to carry the current, and > the other with be a signal trace (carrying no current) that ensures the > voltage drop across just the resistor is sensed - the voltage drop across > power tracks, ground planes etc are ignored. The only tricky stuff with > this is that it requires common-mode input ranges beyond, or at least close > to, the supplies in many situations - but this is no longer rocket science. > I agree with most here except the "carrying no current", where I would say that that there is quite probably at least a small amount current (unless the amplifier has CMOS or FET inputs) but which is nontheless large enough to be affected by the restivity of the trace, where too narrow a trace, or differences in thickness and or width in manufacturing could cause differences in operation of the sensing circuit from board to board. If this is a very high current application, there could even be some fairly decent currents in the feedback loop, depending on just what was going on in the "regulator" portion of the circuit. In many regulator IC's this feedback input can even be the base of a bipolar transistor, whose operation is actually current controlled, notwithstanding that it may appear an amplifier in the datasheet. Even in the case of CMOS or FET inputs to an amplifier, which I think would be avoided in this type of application, but which really would have no current flow involved, I would still maintain that crosstalk and any losses due to restivity should still be avoided. I concurr respecting the 4 connections, but I am simply assuming that the 2 connections on the side of the voltage source (or ground in the sceneario discribed by Abd) are considersd internal to the regulation circuit, and have therefore not discussed them. I am also assumming that there is a regulator circuit involved in the original application which lead to the initial questions in this post, but possibly I am going to far in that assumption, which I have based most of my comments on, and even some here above. Oh well. Thanks for the feedback. JaMi * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
> -Original Message- > From: Ian Wilson [mailto:[EMAIL PROTECTED] > Sent: Thursday, 4 September 2003 13:11 > To: Protel EDA Forum > Subject: Re: [PEDA] Joining 2 different nets keeping seperate > identifiers? > -snip- > > I think, Jami, that you are missing a critical aspect or it > is getting > buried in too much verbage. Sorry if I have just missed it, I > am afraid I > am doing you something of a disservice by not reading your > post(s) in full. > -snip- I hear that. If I had time to read Jami's posts in full I would not be at work! :) * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
On 12:43 PM 4/09/2003, JaMi Smith said: There are basically two different ways that a current sense resistor is normally used. The first is between a voltage source and a "load", and the second is between the "load" and ground. In both cases, the voltage drop is measured across the current sense resistor between the supply leg and the "load". I think, Jami, that you are missing a critical aspect or it is getting buried in too much verbage. Sorry if I have just missed it, I am afraid I am doing you something of a disservice by not reading your post(s) in full. It is common to have four connections to a current sense resistor, two on each side. One on each side will be big and fat to carry the current, and the other with be a signal trace (carrying no current) that ensures the voltage drop across just the resistor is sensed - the voltage drop across power tracks, ground planes etc are ignored. The only tricky stuff with this is that it requires common-mode input ranges beyond, or at least close to, the supplies in many situations - but this is no longer rocket science. Ian * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
Oops, sorry for the empty response . . . that's what happens when you double click the reply button . . . operator error . . . I think that there should be a little more clarification of a few things before the misunderstanding in this thread becomes too rampant. There are basically two different ways that a current sense resistor is normally used. The first is between a voltage source and a "load", and the second is between the "load" and ground. In both cases, the voltage drop is measured across the current sense resistor between the supply leg and the "load". Typically, in this type of scenario, the voltage source is the output of a regulator, with the "feedback" from the "load" side of the current sense resistor being used to control the output of that regulator. My original response and follow-up, as well as my response to Ian's post, are based on a current sense resistor being used between the voltage source and the "load". I believe that Ian's response to my post also assumed that we were talking about the current sense resistor being placed between the voltage source and the "load" also, but it may not have, although it does not really make a difference in his post or in my response to it. It appears that Abd, in his response below, is invisioning the current sense resistor in the second location mentioned above, which is between the "load" and ground, or possibly that could be better understood if it is stated as the between the "return" from the "load" and the ground. While this is different than I envisioned, the problem is really the same, and that is that the current sense resistor is usually put in one leg of a supply or regulator curcuit (either positive or negative) so that the current can be determined by measuring the voltage drop across the resistor between that leg of the supply and the "load", or if you prefer, between the "load" and the supply. In either case, the "feedback" to the amplifier must be connected to the "load" side of the current sense resistor, with the other side of the current sense resistor connected to the appropriate positive or negative source, as dictated by the design requirements of the circuit, such that the current sense resistor is "in series" with the "load" This "load" side of the current sense resistor is both the place that any high currents going to or comming from the "load" must travel in order to get from or to the supply (or regulator circuit), and it is also the place from which a "feedback" trace must be connected back to the input of the amplifier that moniters the voltage drop across the current sense resistor. I am pointing this out so that anyone reading this compilation of responses can understand the differences in the possible location of the current sense resistor in the different discussions, and understand that while there are these differences, the requirements for handling the "feedback" from the "load" side of the current sense resistor is virtually the same in all of the discussions, notwithstanding possible confusion brought about by where the "supply" end of the current sense resistor is located. With that said, I have a few additional comments below. JaMi ----- Original Message - From: "Abd ul-Rahman Lomax" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Wednesday, September 03, 2003 4:50 PM Subject: Re: [PEDA] Joining 2 different nets keeping seperate identifiers? > At 07:09 AM 9/3/2003, Joe McCauley wrote: > >I need to have a current return line with 3mm thickness. This line has a net > >identifier of 'Iret'. > >This line connects to a current sense resistor. I need to take a line from > >this resistor to an amplifier input. > > Here is what I understand from this: this circuit is measuring current by > measuring the voltage drop across the sense resistor. The current being > measured is sufficient that a 3 mm trace is required. Presumably the > temperature rise calculations have been done Or the trace is that fat > so that error due to voltage drop in the trace is minimized. > > >There is no need for this amplifier input line to be 3mm thick, in fact from > >the point of view of routing it would be better if it were not! > > Mr. McCauley writes about one line. Really, there are two, since one is > measuring the voltage drop across a resistor. Of course, if there is a > solid enough ground at the ground side of the sense resistor, one might > assume that the drop in that part of the circuit can be neglected. Or > perhaps the circuit will be calibrated to account for that additional drop. > Otherwise one needs *two* sense lines, which
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
- Original Message - From: "Abd ul-Rahman Lomax" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Wednesday, September 03, 2003 4:50 PM Subject: Re: [PEDA] Joining 2 different nets keeping seperate identifiers? > At 07:09 AM 9/3/2003, Joe McCauley wrote: > >I need to have a current return line with 3mm thickness. This line has a net > >identifier of 'Iret'. > >This line connects to a current sense resistor. I need to take a line from > >this resistor to an amplifier input. > > Here is what I understand from this: this circuit is measuring current by > measuring the voltage drop across the sense resistor. The current being > measured is sufficient that a 3 mm trace is required. Presumably the > temperature rise calculations have been done Or the trace is that fat > so that error due to voltage drop in the trace is minimized. > > >There is no need for this amplifier input line to be 3mm thick, in fact from > >the point of view of routing it would be better if it were not! > > Mr. McCauley writes about one line. Really, there are two, since one is > measuring the voltage drop across a resistor. Of course, if there is a > solid enough ground at the ground side of the sense resistor, one might > assume that the drop in that part of the circuit can be neglected. Or > perhaps the circuit will be calibrated to account for that additional drop. > Otherwise one needs *two* sense lines, which will feed a differential > amplifier of some kind. > > Presumably there will be negligible current in the sense line (the > "amplifier input line.") At least whatever measures that voltage should be > designed to minimize the current. So the line can be narrow, really it only > needs to be wide enough to be reliably fabricated. > > > Is there a > >way of joining 2 different nets in the schematic while keeping seperate > >identifiers? If there were then I could setup the design rules in PCB to > >always have the 'Iret' net 3mm thick, while the other one which connects to > >it could be (say) 0.35mm. Am I over complicating things by trying to do it > >this way? > > I don't think so. I'm from the school that thinks that good DRC is very > important. You can certainly accomplish what you want by setting the > minimum thickness for Iret at 0.35 mm and the maximum at 3 mm. But this > won't guarantee that you get 3 mm where it is needed. > > There might be some way to do this with from-tos, as mentioned by another > designer, but I don't know that. I do notice that From-To Class is one of > the possible attributes controlling width rules, but I've never > investigated that rule. Maybe I should read the manual Naah, that's > something I recommend to others, I don't do it myself :-) > > As mentioned by Mr. Ross, the so-called "virtual short" will accomplish > this. Once you have built this footprint, have placed a symbol for it on > the schematic and have wired it, and have set a design rule for the > footprint (or component class, if by some chance you had different kinds of > these creatures), it is pretty much set and forget. > > You would have your IRet net, being the return net for your large current. > Then you would place, on your schematic, the virtual short, which is, for > schematic purposes, a jumper. One side of the jumper is connected to IRet, > typically right at the sense resistor pad. The other side of the jumper is > connected to your sense net that goes to the amplifier. You could actually > make the jumper structure part of the sense resistor pad, which would > guarantee that the short is placed in the proper location. In other words, > you'd build a symbol and footprint for the sense resistor that had two > extra pads for the sense connections. > > These pads have a gap between them which is below fabrication possibility. > Properly designed, there will actually be *no* gap on the films, because > the gap will be well below the gerber resolution. It might be, say 4 > microinches. (Protel can get a tad flaky in the microinch region since > that's the database resolution, as I recall, otherwise it could be 1 > microinch!) Then a design rule allows pads in that particular footprint to > be very close to each other, say 2 microinches, without creating a DRC > violation. By the way, you'll use rectangular pads > > How do you make the virtual short? I described above the principle for > using fabrication limits to create a physical short that Protel considers > as being unconnected. There is at least one other way, which became > practical and reasonably safe when the CAM Manager was created, all
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
At 07:09 AM 9/3/2003, Joe McCauley wrote: I need to have a current return line with 3mm thickness. This line has a net identifier of 'Iret'. This line connects to a current sense resistor. I need to take a line from this resistor to an amplifier input. Here is what I understand from this: this circuit is measuring current by measuring the voltage drop across the sense resistor. The current being measured is sufficient that a 3 mm trace is required. Presumably the temperature rise calculations have been done Or the trace is that fat so that error due to voltage drop in the trace is minimized. There is no need for this amplifier input line to be 3mm thick, in fact from the point of view of routing it would be better if it were not! Mr. McCauley writes about one line. Really, there are two, since one is measuring the voltage drop across a resistor. Of course, if there is a solid enough ground at the ground side of the sense resistor, one might assume that the drop in that part of the circuit can be neglected. Or perhaps the circuit will be calibrated to account for that additional drop. Otherwise one needs *two* sense lines, which will feed a differential amplifier of some kind. Presumably there will be negligible current in the sense line (the "amplifier input line.") At least whatever measures that voltage should be designed to minimize the current. So the line can be narrow, really it only needs to be wide enough to be reliably fabricated. Is there a way of joining 2 different nets in the schematic while keeping seperate identifiers? If there were then I could setup the design rules in PCB to always have the 'Iret' net 3mm thick, while the other one which connects to it could be (say) 0.35mm. Am I over complicating things by trying to do it this way? I don't think so. I'm from the school that thinks that good DRC is very important. You can certainly accomplish what you want by setting the minimum thickness for Iret at 0.35 mm and the maximum at 3 mm. But this won't guarantee that you get 3 mm where it is needed. There might be some way to do this with from-tos, as mentioned by another designer, but I don't know that. I do notice that From-To Class is one of the possible attributes controlling width rules, but I've never investigated that rule. Maybe I should read the manual Naah, that's something I recommend to others, I don't do it myself :-) As mentioned by Mr. Ross, the so-called "virtual short" will accomplish this. Once you have built this footprint, have placed a symbol for it on the schematic and have wired it, and have set a design rule for the footprint (or component class, if by some chance you had different kinds of these creatures), it is pretty much set and forget. You would have your IRet net, being the return net for your large current. Then you would place, on your schematic, the virtual short, which is, for schematic purposes, a jumper. One side of the jumper is connected to IRet, typically right at the sense resistor pad. The other side of the jumper is connected to your sense net that goes to the amplifier. You could actually make the jumper structure part of the sense resistor pad, which would guarantee that the short is placed in the proper location. In other words, you'd build a symbol and footprint for the sense resistor that had two extra pads for the sense connections. These pads have a gap between them which is below fabrication possibility. Properly designed, there will actually be *no* gap on the films, because the gap will be well below the gerber resolution. It might be, say 4 microinches. (Protel can get a tad flaky in the microinch region since that's the database resolution, as I recall, otherwise it could be 1 microinch!) Then a design rule allows pads in that particular footprint to be very close to each other, say 2 microinches, without creating a DRC violation. By the way, you'll use rectangular pads How do you make the virtual short? I described above the principle for using fabrication limits to create a physical short that Protel considers as being unconnected. There is at least one other way, which became practical and reasonably safe when the CAM Manager was created, allowing custom CAM setups for your design. One of the mech layers is dedicated to a short, that is, a shorting trace is on that mech layer. It is merged with the normal layer as part of the CAM definition for the normal layer. With the fabrication limit method, you need to create a design rule. It's a good thing that if you forget to do this, you will get a DRC error, so this is quite safe. The down side of this method is that if you aren't careful about how your CAM pad definitions are created, roundoff can leave a real gap on the film and a helpful fabricator will increase it for you, this has actually happened. The mech layer merge technique will produce a bulletproof fab film, but if you forget to create the CAM definitio
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
Ian, Please see below, JaMi - Original Message - From: "Ian Wilson" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Wednesday, September 03, 2003 3:49 PM Subject: Re: [PEDA] Joining 2 different nets keeping seperate identifiers? > On 07:40 AM 4/09/2003, JaMi Smith said: > >Joe, > > > >Who says it has to be a "3mm thickness" (I think you may actually mean that > >the trace has to be 3 mm wide)? > > > >Is this requirement imposed on you by an Engineer, or is it some requirement > >found in a datasheet for some specific circuit or device? > > I would expect that the spec is wide uncalibrated current carrying traces > with narrow current *sense* traces running off to the sense > amplifier. This is a pretty standard sort of interface in high or > precision voltage or current applications. You take a pair of sense traces > to the load or sense resistor rather than using the uncalibrated high > current traces for both current carrying and sensing. The 3mm width > requirement would come from the expected current, while the thinner traces > are used for the actual sensing. Very standard stuff. > > (Many bench-top power supplies will have sense terminals that allow you to > control the voltage at the load rather than at the supply terminals, there > is usually weak feedback in the supply to ensure that the supply is > controlled if the sense terminals are unconnected.) > > The requirement is perfectly reasonable to me and I would either solve it > by setting up from-tos and appropriate rules or by the Lomax Virtual > short. In DXP it could be solved by a net tie component. > > Ian > The initial question is not because I want or need to know why there is a requirement for a 3 mm trace width, but so that Joe can understand what the problem is, and just what the requirement may apply to. While I wouldn't necessarily state what you did in your first paragraph the way that you stated it, it does get the point across, and is not different than mine (although stated somewhat backwards as compared to what I stated). If you will carefully re-read my post, and also read the follow-up post with what I forgot to put in the original, you will see that I am trying to explain just where the high current is and where it goes, and just exactly what the current sense resistor does, and what the requirements may be for a "feedback" trace from the "load" side of that current sense resistor, and what the 3 mm requirement may apply to. If you will also carefully re-read the original post from Joe, you will see that this requirement has nothing to do with remote sensing, such as in your example in your second paragraph of the power supply, but that he is directly taking a trace from the "load" side of the current sense resistor, and feeding it directly back into the [current sense] amplifier input. I am sorry for my omission in my original post, but hopefully with the supplement from my follow-up post, it will all become clear. Yes, my original post is a bit confusing, but I think that you will see that we are saying the pretty much same thing, with respect to your first paragraph above, and that your second paragraph really does not apply to this instance. Respecting your last paragraph, I am fairly sure that when you get my follow-up post and think the whole thing thru together with the first post, that you would concurr with me in what I stated in my follow-up post, that the present case that Joe is describing, that the "feedback" trace is in fact the same "net" as the "net" connected to the "load" side of the current sense resistor (which in fact is just exactly what you yourself describe in your first paragraph above), and that it really should not have a different "net" name, and that the different net name is the real problem here (but which would not be the case in the example of your second paragraph). That said, I think that you would additionally concurr with my stating that anything that would introduce any "loss" or "drop" in the "feedback" trace should be avoided (such as the loss that would almost certainly be introduced by unnecessarily using 2 differnt net names and trying to join it all together with a "Lomax Virtual Short" (with its intentional gap which can allow for some small and uncontrolled amount of etching of the trace at the point of the gap), or by using too narrow a trace which could cause too much restivity in the trace). I would also think that whatever DXP may or may not do here does nothing but confuse the issue (especially if there is no reason to have 2 different nets in the first place). Sorry for any confusion, but I think you may be trying to say the same thing as I did with respe
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
On 07:40 AM 4/09/2003, JaMi Smith said: Joe, Who says it has to be a "3mm thickness" (I think you may actually mean that the trace has to be 3 mm wide)? Is this requirement imposed on you by an Engineer, or is it some requirement found in a datasheet for some specific circuit or device? I would expect that the spec is wide uncalibrated current carrying traces with narrow current *sense* traces running off to the sense amplifier. This is a pretty standard sort of interface in high or precision voltage or current applications. You take a pair of sense traces to the load or sense resistor rather than using the uncalibrated high current traces for both current carrying and sensing. The 3mm width requirement would come from the expected current, while the thinner traces are used for the actual sensing. Very standard stuff. (Many bench-top power supplies will have sense terminals that allow you to control the voltage at the load rather than at the supply terminals, there is usually weak feedback in the supply to ensure that the supply is controlled if the sense terminals are unconnected.) The requirement is perfectly reasonable to me and I would either solve it by setting up from-tos and appropriate rules or by the Lomax Virtual short. In DXP it could be solved by a net tie component. Ian * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
Joe, Oops !!! I actually forgot to the most important statement in my whole response, although it is implied (I actually started to write it in one place, but changed it and wrote something else, and then forgot to put it back in another location). The net name of the "feedback" trace, which in your case you said is "Iret", must (as in ABSOLUTELY MUST) have the identical (as in ABSOLUTELY IDENTICAL) net name as anything and everything else connectet to the "load" side of the current sense resistor. It >>> IS <<To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Wednesday, September 03, 2003 4:09 AM Subject: [PEDA] Joining 2 different nets keeping seperate identifiers? > I need to have a current return line with 3mm thickness. This line has a net > identifier of 'Iret'. > This line connects to a current sense resistor. I need to take a line from > this resistor to an amplifier input. > There is no need for this amplifier input line to be 3mm thick, in fact from > the point of view of routing it would be better if it were not! Is there a > way of joining 2 different nets in the schematic while keeping seperate > identifiers? If there were then I could setup the design rules in PCB to > always have the 'Iret' net 3mm thick, while the other one which connects to > it could be (say) 0.35mm. Am I over complicating things by trying to do it > this way? > > Thanks for any pointers, > > Joe > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
Joe,
Who says it has to be a "3mm thickness" (I think you may actually mean that
the trace has to be 3 mm wide)?
Is this requirement imposed on you by an Engineer, or is it some requirement
found in a datasheet for some specific circuit or device?
A "current sense resistor" has to be "in series" ("in line" like a fuse
would be) with the "load" (the circuit or voltage that is being sensed) so
that it can determine how much current is being used. In most cases a
current sense resistor is used so that there can be some "feedback" to the
circuit that is controlling the voltage output of some type of voltage
regulator (or voltage distribution), however, in few cases, it may be used
so that the current can be measured for some other reason such as to take a
measurement for a remote "monitor" of some kind.
In most, if not all cases, there needs to be a direct and unobstructed path
back to the "feedback" input of the controlling circuit (which in your case
is the amplifier input) which has no additional "loss" (such as a "resistive
drop" in the trace) which could otherwise affect the measurement. Typically,
this requirement may be met by specifying a wide trace (such as your 3 mm
requirement) for the "feedback" signal, but more often, a very short and
direct trace can be used, which can usually be accomplished by having a
good component placement so that the current sense resistor is not too far
away from the circuit involved (however, you must still watch out for any
"direct" "feedback" to the amplifier input from the other end of the current
sense resistor, which is usually the "output" of the "controlling" circuit
(in other words, the location of the sense resistor can be very critical)).
As stated above, the current sense resistor is "in series" with the "load",
and this means that it is only there so that you can measure the current
going thru it (by forcing a very small and controlled amount of current
"limiting"), as opposed to being in the circuit for some other kind of
current "limiting", which is the normal function of a resistor. This means
that the "load" side of the sense resistor (where you are also taking the
trace back to the amplifier input (for a feed back measurement)) is also in
most cases the "supply" voltage for whatever circuit is connected to this
"load" side of the current sense resistor. This would mean that it should be
a wider than normal trace so that it can handle the "power distribution" to
that circuit, just as if it were the normal "VCC" (or other power supply)
trace in your circuit if you were not using any internal planes for power or
ground distribution.
With that said, the real question that needs to be addressed here is just
how much current is going thru the sense resistor to the "load".
It may just be that the 3 mm requirement in your case is for the "load"
itself, as opposed to the "feedback" line from the "load".
On the other hand, if there is a very large "load" (on the "output side of
the current sense resistor) that is being "measured" by the "feedback"
trace, then 3 mm might be a very appropriate width for the trace.
What is critical here, is that you do not want any "loss" or any other
"variables" in this "feedback" trace (which would affect the "feedback"
measurement) that may vary from board to board due to such things as
manufacturing processes (etching or plating differences or minute
differences it the copper (trace) thickness), or which may vary in the same
board from such things as the resistivity of the trace varying due to
changes in ambient temperature during operation.
All of this boils down to having a very good and direct path back to the
"current sensing" input of the amplifier in your application which will not
have any resistive "loss" or "drop".
Thus the 3 mm width requirement.
In this case, I would additionally say that you do not want to have any
feedthrus or vias in this "feedback" trace, nor do you want to have anything
else in the trace that might in someway affect the resistivity of the trace.
A parallel response to this post, which deals with your wanting to use two
"2 different nets" (the subject of this thread), suggests that you might be
able to use two different nets as you request in your original post, and
then using the "Lomax Virtual Short" method to join your two 2 different
nets together. This would be a very good solution to your problem in just
about any other application but this one, since the "Virtual Short" plays
some tricks on Protel by having a very very small gap between the traces to
overcome DRC errors and objections, but which itself is reliant on the two
traces actually "bridging" or "shorting" the small gap (or more accurately,
not etching it thru completely, or bridging it with solder) during the
manufacturing of the board, which unquestionably will have a major impact on
the actual "resistivity" of the "feedback" trace involved. For this reason,
I would strongly advise you to not use the "Lomax Virtual S
Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
> -Original Message- > From: Joe McCauley [mailto:[EMAIL PROTECTED] > Sent: Wednesday, September 03, 2003 12:10 PM > To: Protel EDA Forum > Subject: [PEDA] Joining 2 different nets keeping seperate identifiers? > > > I need to have a current return line with 3mm thickness. This > line has a net identifier of 'Iret'. This line connects to a > current sense resistor. I need to take a line from this > resistor to an amplifier input. There is no need for this > amplifier input line to be 3mm thick, in fact from the point > of view of routing it would be better if it were not! Is > there a way of joining 2 different nets in the schematic > while keeping seperate identifiers? If there were then I > could setup the design rules in PCB to always have the 'Iret' > net 3mm thick, while the other one which connects to it could > be (say) 0.35mm. Am I over complicating things by trying to > do it this way? Joe Mr Lomax had a method to do this as a 'virtual short', a feature now supported in DXP called 'net ties'. If you browse the archive you will find it. But if this is a once only route, then you may find it less time intensive just to do this route by hand. Have you tried defining the 'from to' topology and applying a width rule with filter set to from-to? Just an idea. Best Regards John A. Ross RSD Communications ltd Email [EMAIL PROTECTED] WWWhttp://www.rsd.tv == * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
